CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Meshing & Mesh Conversion (http://www.cfd-online.com/Forums/openfoam-meshing/)
-   -   Multiple internal wall an fluid zones (http://www.cfd-online.com/Forums/openfoam-meshing/92250-multiple-internal-wall-fluid-zones.html)

miles_davis September 7, 2011 13:39

Multiple internal wall an fluid zones
 
Hi Foamer
I am trying to convert a .msh file with multiple internal walls.
After many try I have managed to reproduce the procedure from the open wiki
http://openfoamwiki.net/index.php/Ho...internal_walls

I have some problems and questions
Firsts this procedure did note worked on a 2D quad mesh.
When I do the checkMesh I have 3 kinds of error :


Checking topology...
Boundary definition OK.
***Total number of faces on empty patches is not divisible by the number of cells in the mesh. Hence this mesh is not 1D or 2D. :confused:
Cell to face addressing OK.
***Unused points found in the mesh, number unused by faces: 2 number unused by cells: 2 :confused:
<<Writing 2 unused points to set unusedPoints
Upper triangular ordering OK.
Face vertices OK.
Number of regions: 1 (OK).
Checking patch topology for multiply connected surfaces ...
Patch Faces Points Surface topology
entre_eau_brute 63 128 ok (non-closed singly connected)
sortie_eau 32 66 ok (non-closed singly connected)
degazage 250 502 ok (non-closed singly connected)
surf_base_buse 16 34 ok (non-closed singly connected)
wall 655 1316 ok (non-closed singly connected)
frontAndBackPlanes 184008 185324 ok (non-closed singly connected)
real-wall_buse_1 148 302 ok (non-closed singly connected)
real-wall_buse_2 150 304 ok (non-closed singly connected)
Checking geometry...
Overall domain bounding box (-4.44089e-16 0 -0.0282843) (2 2 0.0282843)
Mesh (non-empty, non-wedge) directions (0 0 0)
Mesh (non-empty) directions (0 0 0)
***Number of edges not aligned with or perpendicular to non-empty directions: 360577 :confused:
<<Writing 184185 points on non-aligned edges to set nonAlignedEdges
***Boundary openness (8.32459e-07 1.86471e-06 1.49086e-19) possible hole in boundary description. :confused:
***Open cells found, max cell openness: 0.333333, number of open cells 2 :confused:
<<Writing 2 non closed cells to set nonClosedCells
Minumum face area = 2.83025e-06. Maximum face area = 0.000622352. Face area magnitudes OK.
Min volume = 1.60104e-07. Max volume = 5.96973e-06. Total volume = 0.226274. Cell volumes OK.
Mesh non-orthogonality Max: 28.4768 average: 1.40368
Non-orthogonality check OK.
Face pyramids OK.
Max skewness = 0.750378 OK.




My second concern is when I try to apply the procedure to a multiple internal-wall mesh.
I start with one of the internal wall.
A new folder is created named 0.001.
Inside I can find all the file corresponding to the new mesh.
But I don't have any Sets folder as in the constant folder where the original mesh is still located.
In the wiki it is indicated to use the instruction SplitMeshWithSets .
The problem is that I am using OF 2.01 and this instruction is not available anymore.:eek:
My question can be resume in How can I apply several times the SplitMesh procedure on a given mesh :confused:


Third question,
Can OF handle a mesh with multiple Fluid zone as in fluent.
I am looking for a tuto on the subject. Has anyone some resource on the subject?


Thanks a lot for you help.


Regards,


Miles

gschaider September 7, 2011 14:27

Quote:

Originally Posted by miles_davis (Post 323317)
Hi Foamer
I am trying to convert a .msh file with multiple internal walls.
After many try I have managed to reproduce the procedure from the open wiki
http://openfoamwiki.net/index.php/Ho...internal_walls

That page is hopelessly outdated (as you can see from the tags). I hope that you update it should you find a solution

Quote:

Originally Posted by miles_davis (Post 323317)
I have some problems and questions
Firsts this procedure did note worked on a 2D quad mesh.
When I do the checkMesh I have 3 kinds of error :


Checking topology...
Boundary definition OK.
***Total number of faces on empty patches is not divisible by the number of cells in the mesh. Hence this mesh is not 1D or 2D. :confused:
Cell to face addressing OK.
***Unused points found in the mesh, number unused by faces: 2 number unused by cells: 2 :confused:
<<Writing 2 unused points to set unusedPoints
Upper triangular ordering OK.
Face vertices OK.
Number of regions: 1 (OK).
Checking patch topology for multiply connected surfaces ...
Patch Faces Points Surface topology
entre_eau_brute 63 128 ok (non-closed singly connected)
sortie_eau 32 66 ok (non-closed singly connected)
degazage 250 502 ok (non-closed singly connected)
surf_base_buse 16 34 ok (non-closed singly connected)
wall 655 1316 ok (non-closed singly connected)
frontAndBackPlanes 184008 185324 ok (non-closed singly connected)
real-wall_buse_1 148 302 ok (non-closed singly connected)
real-wall_buse_2 150 304 ok (non-closed singly connected)
Checking geometry...
Overall domain bounding box (-4.44089e-16 0 -0.0282843) (2 2 0.0282843)
Mesh (non-empty, non-wedge) directions (0 0 0)
Mesh (non-empty) directions (0 0 0)
***Number of edges not aligned with or perpendicular to non-empty directions: 360577 :confused:
<<Writing 184185 points on non-aligned edges to set nonAlignedEdges
***Boundary openness (8.32459e-07 1.86471e-06 1.49086e-19) possible hole in boundary description. :confused:
***Open cells found, max cell openness: 0.333333, number of open cells 2 :confused:
<<Writing 2 non closed cells to set nonClosedCells
Minumum face area = 2.83025e-06. Maximum face area = 0.000622352. Face area magnitudes OK.
Min volume = 1.60104e-07. Max volume = 5.96973e-06. Total volume = 0.226274. Cell volumes OK.
Mesh non-orthogonality Max: 28.4768 average: 1.40368
Non-orthogonality check OK.
Face pyramids OK.
Max skewness = 0.750378 OK.




My second concern is when I try to apply the procedure to a multiple internal-wall mesh.
I start with one of the internal wall.
A new folder is created named 0.001.
Inside I can find all the file corresponding to the new mesh.
But I don't have any Sets folder as in the constant folder where the original mesh is still located.
In the wiki it is indicated to use the instruction SplitMeshWithSets .
The problem is that I am using OF 2.01 and this instruction is not available anymore.:eek:
My question can be resume in How can I apply several times the SplitMesh procedure on a given mesh :confused:

Check out the createBaffles utility. I haven't used it, but it uses faceZones instead of sets which should be preserved

Quote:

Originally Posted by miles_davis (Post 323317)
Third question,
Can OF handle a mesh with multiple Fluid zone as in fluent.
I am looking for a tuto on the subject. Has anyone some resource on the subject?

What do you need the multiple zones for? Answer depends on that

miles_davis September 7, 2011 17:22

Hi

Thanks for your answer.

Concerning the procedure described in the wiki, I agree that it looks outdated. The thing is that's the only source I had so far.
I am gonna search the web for a tutorial on the utility you have just mentioned. Thanks for that.
Note that the procedure seems to work as long as you only have one internal wall. So it was helpful as a start.

I want to have many fluid zones for a lot of reason.
I intend to do a multiphase simulation. And sometimes it is useful to have a full area in Witch you can impose velocity and volume fraction, instead of having just a surface inlet.
Besides i want to do some MRF calculation in the future so according to my Fluent experience it might be useful to be able to set different condition in different fluid zone. But I am a OF beginner so maybe it is not necessary.
Any advices are welcome.

Thanks again.

P.S.: Do you know if the createBaffles utility work with both tri, quad or even mixed meshes?

miles_davis September 8, 2011 06:53

p { margin-bottom: 0.21cm; }

Hi again,


I want to try the Createbaffle utility but I don't find any example on the subject.

Does anyone have any source or documentation please?


On the OF wiki I have found the user utility
http://openfoamwiki.net/index.php/Co...mWithInternals
It comes with a source code;
do you know How i install additional codes on OF 2.0.?

Last question I know this my sound wired but I have difficulties to understand the exact definition of some basic OF notion.
In your advice you said " it uses faceZones instead of sets which should be preserved"


What is a Set exactly
What is the difference between a set and a zone.

Therefore I should be able to understand the full meaning of your advice.

Please do not doubt i have search the UG and in the Forum but people seem so familiar with the usual OF terms so it is hard to catch the train in motion.:(


Thanks for any help

gschaider September 8, 2011 09:26

Quote:

Originally Posted by miles_davis (Post 323389)
p { margin-bottom: 0.21cm; }

Hi again,


I want to try the Createbaffle utility but I don't find any example on the subject.

Does anyone have any source or documentation please?

Documentation: not more than what you get with the -help/-doc/-srcDoc options of the command (and least what I know)

Source should be at $FOAM_UTILITIES/mesh/manipulation

Quote:

Originally Posted by miles_davis (Post 323389)
On the OF wiki I have found the user utility
http://openfoamwiki.net/index.php/Co...mWithInternals
It comes with a source code;
do you know How i install additional codes on OF 2.0.?

Forget this version:
a) it won't compile with 2.0
b) that functionality is in the regular fluentMeshToFoam since a long time ago (check with -help)

Quote:

Originally Posted by miles_davis (Post 323389)
Last question I know this my sound wired but I have difficulties to understand the exact definition of some basic OF notion.
In your advice you said " it uses faceZones instead of sets which should be preserved"

What is a Set exactly
What is the difference between a set and a zone.

Therefore I should be able to understand the full meaning of your advice.

This has been discussed elsewhere on the forum. Look for cellSet and cellZone (or faceSet and faceZone)

Quote:

Originally Posted by miles_davis (Post 323389)
Please do not doubt i have search the UG and in the Forum but people seem so familiar with the usual OF terms so it is hard to catch the train in motion.:(

You're venturing into the regions of OF that are not over-documented. I know that is hard.

miles_davis September 8, 2011 14:56

p { margin-bottom: 0.21cm; } Hi


I complete this thread with the method I have built in order to make multiple baffle definition.
Please note that I am starting from a 2D mesh generated with TGRID or ANSYS MESHING.
The file was of course in ASCII format.


Step1
fluentMeshToFoam <case> -writeSets
you'll get a mesh with a Sets folder including all the sets corresponding to all the surfaces inside your initial mesh
I also get the Zones files but they were empty
Step2
setsToZones -noFlipMap
This will fill the Zones files that were empty after the first conversion
Step3
Go in the boundary file and add 2 patches for the future pacth generated by the creation of the baffle
add the line
toto_1{
type wall;
nFaces 0;
startFace xxx;
}
toto_2
{
type wall;
nFaces 0;
startFace xxx;
}
To get the number xxx just sum the number of faces of the last patch of your boundary file (before change of course) with the number startFace for this patch.
N.B. : Do not forget to update the total number of patches at the beginnig of your boundary file since you are adding 2 new patches
Step4
Add the boundary condition for a wall for the two new patches in the 0/ folder
Step5
createBaffles -overwrite tata "(toto_1 toto_2)"
tata is the name of the surface you want to convert into a baffle (it should be listed in your faceZones file or in the list of the file in your sets directory)


You can repeat the procedure starting from step3 for every baffle you want to create


N.B. : There is an option -additionalPatches that seems to avoid you to modify the boundary file yourself but I did not manage to make it work




If you have something more straightforward than the heavy procedure I would love to know it.:)




I will try on a 3D mesh to see if the baffle conversion is automatic and if not if this procedure works as well.

Attesz April 25, 2012 07:36

Hi Miles,

thanks for the description. Did you try it finally on 3D cases?

I want to do the procedure on a fan geometry.

Best,
Attila

miles_davis April 25, 2012 07:47

Hi,

It's been a while since I last digged in OF meshing conversion problems.
But you can be sure that with a 3D geometry there is no need to worry about baffles: The baffles present in your geometry will automatically be conserved during the mesh conversion.
Fluent3DMeshToFoam <case>
If you want to keep the different fluid zones you may have defined in your mesh, use the -writeSets option.

Regards,


Miles

Attesz April 25, 2012 07:49

Okay, thank you!

Have a nice day,
Attila

PonchO July 17, 2012 06:09

Hiho Foamers,

I have a problem by using createBaffles to make internal walls with zero-thickness.

OF-2.0.x

My Case works as follows (just to give an overview):
I have 5 Chambers divided by a very thin wall and from chamber to chamber a slot is in an alternating fashion left at the top or at the bottom of the chamber.
On the bottom of each chamber is an inlet and an the top is the outlet.

I will define each wall as a faceSet and then into a faceZone in the topoSetDict (and later with createBaffles as a boundary with zero thickness).

Code:

actions
(
    //set faceSet and faceZone of Wall1
    {
            name    internalWall1;
            type    faceSet;
            action  new;
            source boxToFace;
        sourceInfo
            {
                box  (0.10199 0 0.055) (.1021 0.15 0.25);
          }
        }
   
    {
        name internalWallZone1;
        type faceZoneSet;
        action new;
        source setToFaceZone;
        sourceInfo
            {
                set internalWall1;
            faceSet internalWall1;
          }
    }
    //set faceSet and faceZone of Wall2
    {
            name    internalWall2;
            type    faceSet;
            action  new;
            source boxToFace;
        sourceInfo
            {
                box  (0.20399 0 0) (0.20401 0.15 0.25);
          }
        }
   
    {
        name internalWallZone2;
        type faceZoneSet;
        action new;
        source setToFaceZone;
        sourceInfo
            {
                set internalWall2;
            faceSet internalWall2;
          }
    }
//and so on...

this works fine and topoSet delivers the faceZones.

But if i will run createBaffles for the first internal wall with:
createBaffles internalWallZone1 '(internalWall1 internalWall1)'

i get an output of createBaffles ending with an error-message:

Code:

Create time

Create mesh for time = 0

Converting faces on zone "internalWallZone1" into baffles.

Found 100 faces on zone "internalWallZone1"

Using master patch internalWall1 at index 11
Using slave patch internalWall1 at index 11
Reading geometric fields

Reading volScalarField alphat
Reading volScalarField p
Reading volScalarField T
Reading volScalarField k
Reading volScalarField epsilon
Reading volScalarField mut
Reading volVectorField U
#0  Foam::error::printStack(Foam::Ostream&) in "/app2/OpenFOAM/OpenFOAM-2.0.x/platforms/linux64Gcc46DPOpt/lib/libOpenFOAM.so"
#1  Foam::sigSegv::sigHandler(int) in "/app2/OpenFOAM/OpenFOAM-2.0.x/platforms/linux64Gcc46DPOpt/lib/libOpenFOAM.so"
#2  in "/lib/libc.so.6"
#3  Foam::List<int>::operator=(Foam::UList<int> const&) in "/app2/OpenFOAM/OpenFOAM-2.0.x/platforms/linux64Gcc46DPOpt/bin/createBaffles"
#4  Foam::polyTopoChange::addFace(Foam::face const&, int, int, int, int, int, bool, int, int, bool) in "/app2/OpenFOAM/OpenFOAM-2.0.x/platforms/linux64Gcc46DPOpt/lib/libdynamicMesh.so"
#5  Foam::polyTopoChange::addMesh(Foam::polyMesh const&, Foam::List<int> const&, Foam::List<int> const&, Foam::List<int> const&, Foam::List<int> const&) in "/app2/OpenFOAM/OpenFOAM-2.0.x/platforms/linux64Gcc46DPOpt/lib/libdynamicMesh.so"
#6  Foam::polyTopoChange::polyTopoChange(Foam::polyMesh const&, bool) in "/app2/OpenFOAM/OpenFOAM-2.0.x/platforms/linux64Gcc46DPOpt/lib/libdynamicMesh.so"
#7 
 in "/app2/OpenFOAM/OpenFOAM-2.0.x/platforms/linux64Gcc46DPOpt/bin/createBaffles"
#8  __libc_start_main in "/lib/libc.so.6"
#9  Foam::UOPstream::write(char) in "/app2/OpenFOAM/OpenFOAM-2.0.x/platforms/linux64Gcc46DPOpt/bin/createBaffles"
Speicherzugriffsfehler

Speciherzugriffsfehler means Segmentation Fault to be clear...
It seems that the error occur corresponding to the U-File, but i don't find anything odd there:

Code:

dimensions      [0 1 -1 0 0 0 0];

internalField  uniform (0 0 0);

boundaryField
{
    internalWall1
    {
        type            fixedValue;
        value          uniform (0 0 0);
    }

    internalWall2
    {
        type            fixedValue;
        value          uniform (0 0 0);
    }

    internalWall3
    {
        type            fixedValue;
        value          uniform (0 0 0);
    }

    internalWall4
    {
        type            fixedValue;
        value          uniform (0 0 0);
    }
   
    wallsFrontBackSide
    {
        type            fixedValue;
        value          uniform (0 0 0);
    }

    inletCh1
    {
        type            fixedValue;
        value          uniform (0 0 16.5);
    }

    inletCh2
    {
        type            fixedValue;
        value          uniform (0 0 23.3);
    }

    inletCh3
    {
        type            fixedValue;
        value          uniform (0 0 13.2);
    }

    inletCh4
    {
        type            fixedValue;
        value          uniform (0 0 23.5);
    }

    inletCh5
    {
        type            fixedValue;
        value          uniform (0 0 10.0);
    }

    outletCh1
    {
        type            zeroGradient;//pressureInletOutletVelocity;
        //value          uniform (0 0 0);
    }

    outletCh2
    {
        type            zeroGradient;//pressureInletOutletVelocity;
        //value          uniform (0 0 0);
    }

    outletCh3
    {
        type            zeroGradient;//pressureInletOutletVelocity;
        //value          uniform (0 0 0);
    }

    outletCh4
    {
        type            zeroGradient;//pressureInletOutletVelocity;
        //value          uniform (0 0 0);
    }

    outletCh5
    {
        type            zeroGradient;//pressureInletOutletVelocity;
        //value          uniform (0 0 0);
    }
}

in the boundary-File i have definied my new patches like this:

Code:

    internalWall1
    {
        type            wall;
        nFaces          100;
        startFace      78950;
    }

    internalWall2
    {
        type            wall;
        nFaces          100;
        startFace      79050;
    }

    internalWall3
    {
        type            wall;
        nFaces          100;
        startFace      79150;
    }

    internalWall4
    {
        type            wall;
        nFaces          100;
        startFace      79250;
    }

I'm working just a short time with OpenFOAM, so i can't figure out what i should try in further operations to accomplish with my case.
Can anybody help me :confused:?

styleworker November 20, 2012 09:28

Hej miles,

thank you for your instructions. It also works for gmshToFoam!


All times are GMT -4. The time now is 14:00.